You can use DEFINE_TURBULENT_VISCOSITY to specify a custom turbulent viscosity function for the Spalart-Allmaras, -
, and
-
turbulence models for single-phase
applications. In addition, for 3D versions of ANSYS Fluent you can specify
a subgrid-scale turbulent viscosity UDF for the large eddy simulation
model. For Eulerian multiphase flows, turbulent viscosity UDFs can
be assigned on a per-phase basis, and/or to the mixture, depending
on the turbulence model. See Table 2.7: Eulerian Multiphase Model and
DEFINE_TURBULENT_VISCOSITY UDF Usage for details.
Table 2.7: Eulerian Multiphase Model and DEFINE_TURBULENT_VISCOSITY UDF Usage
|
Turbulence Model |
Phase that Turbulent Viscosity UDF Is Specified On |
|---|---|
|
|
mixture, primary and secondary phases |
|
|
primary and secondary phases |
|
|
primary and secondary phases |
DEFINE_TURBULENT_VISCOSITY (name, c, t)
|
Argument Type |
Description |
|---|---|
|
|
UDF name. |
|
|
Cell index. |
|
|
Pointer to cell thread on which the turbulent viscosity is to be applied. |
Function returns
real
There are three arguments to DEFINE_TURBULENT_VISCOSITY: name, c, and
t. You supply name, the name of the UDF. c and t are variables that are passed by the ANSYS Fluent solver
to your UDF. Your UDF will need to return the real value of the turbulent viscosity to the solver.
The following UDF, named user_mu_t,
defines a custom turbulent viscosity for the standard -
turbulence model. Note
that the value of
M_keCmu in the example
is defined through the graphical user interface, but made accessible
to all UDFs. The source code can be interpreted or compiled in ANSYS Fluent.
/********************************************************************
UDF that specifies a custom turbulent viscosity for standard
k-epsilon formulation
*********************************************************************/
#include "udf.h"
DEFINE_TURBULENT_VISCOSITY(user_mu_t,c,t)
{
real mu_t;
real rho = C_R(c,t);
real k = C_K(c,t);
real d = C_D(c,t);
mu_t = M_keCmu*rho*SQR(k)/d;
return mu_t;
}
/********************************************************************
Custom turbulent viscosity functions for each phase and the
mixture in a two-phase multiphase flow
*********************************************************************/
#include "udf.h"
DEFINE_TURBULENT_VISCOSITY(mu_t_ke_mixture, c, t)
{
real mu_t;
real rho = C_R(c,t);
real k = C_K(c,t);
real d = C_D(c,t);
real cmu = M_keCmu;
mu_t = rho*cmu*k*k/d;
return mu_t;
}
DEFINE_TURBULENT_VISCOSITY(mu_t_ke_1, c, t)
{
Thread *tm = lookup_thread_by_id(DOMAIN_SUPER_DOMAIN(THREAD_DOMAIN(t)),t->id);
CACHE_T_SV_R (density, t, SV_DENSITY);
CACHE_T_SV_R (mu_t, t, SV_MU_T);
CACHE_T_SV_R (density_m, tm, SV_DENSITY);
CACHE_T_SV_R (mu_t_m, tm, SV_MU_T);
return density[c]/density_m[c]*mu_t_m[c];
}
DEFINE_TURBULENT_VISCOSITY(mu_t_ke_2, c, t)
{
Thread *tm = lookup_thread_by_id(DOMAIN_SUPER_DOMAIN(THREAD_DOMAIN(t)),t->id);
CACHE_T_SV_R (density, t, SV_DENSITY);
CACHE_T_SV_R (mu_t, t, SV_MU_T);
CACHE_T_SV_R (density_m, tm, SV_DENSITY);
CACHE_T_SV_R (mu_t_m, tm, SV_MU_T);
return density[c]/density_m[c]*mu_t_m[c];
}
After the UDF that you have defined using DEFINE_TURBULENT_VISCOSITY is interpreted (Interpreting UDFs)
or compiled (Compiling UDFs), the function
name(s) that you specified in the DEFINE macro
argument(s) (for example user_mu_t for single
phase, or mu_t_ke_mixture, mu_t_ke_1, and mu_t_ke_2 for multiphase) will become
visible and selectable in the Viscous Model dialog
box in ANSYS Fluent. See Hooking DEFINE_TURBULENT_VISCOSITY UDFs for details.